Modal Stress Recovery

The benefit of this process is being able to recover any type of output that is available in MSC.Nastran (also MD Nastran) such as element stresses or strains, nodal forces, and so on. Due to limitations of the MNF, only grid point stresses or strains can be post-processed in Adams. Also, MSC.Nastran does not allow grid point stress or strain on composite shell elements or beams, so it is not possible to post-process strain or stress for these type of elements in Adams. In addition, plates or shells have more than one layer, but the MNF allows only one layer of stress or strain to be stored in the file. These limitations are avoided by exporting data for MSC.Nastran.

MSC.Nastran has the function to recover stresses and strains in the version 2006 (MDR1) and later, and a special DMAP is not required. For modal stress recovery, a restart run is used thus MSC.Nastran database (.MASTER and .DBALL) have to be kept in the primary run to build the flexible body for Adams, and to do that the command option "scratch=no" should be applied. Modal transient response analysis (SOL 112) and modal frequency response analysis (SOL 111) should be applied for time dependent data and frequency dependent data respectively with ADMPOST parameter.

Learn Exporting Data for NASTRAN.

A restart MSC.Nastran for modal stress recovery needs to be specified at the top of the MSC.Nastran input deck in the file management section:

where <logical name> is the logical name of the database to be assigned and <database name> is MASTER file name of the primary run. Note that the logical name is arbitrary characters within 8 letters and first one should be alphabet.

Modal deformations to be read have to be in binary (OUTPUT2) format, and the following statement needs to be specified near the top of the MSC.Nastran input deck in the file management section:

where <MDFilename> is the name of the modal deformations file from Adams. For directions on how to create this file, see the FEMDATA or OUTPUT Adams Solver statement. And <load ID> indicates an ID number of DLOAD statements in the case control section. The option FORM may be requested when the binary format of MDF is not applicable to the platform of MSC.Nastran (see the MSC.Nastran quick reference guide for more information).

Dynamic stress/strain output can be either in F06, PUNCH OUT, XDB or OUTPUT2 according to standard MSC.Nastran functionality, and the output files can be postprocessed in Patran or SimXpert Structures.

If displacements, stresses, and/or strains are to be available for postprocessing, one or more of the following statements must appear in the case control section of the MSC.Nastran input file:

where <load id> is a ID number indicated by ASSIGN statement in the executive control section, and <set id> is a ID number defined in SET statement.

Request modal stress recovery (see the MSC.Nastran quick reference guide for more information):

This parameter is used to activate modal stress recovery and control the addition of rigid body motion with modal deformations. Rigid body motions from an Adams simulation are included in the modal deformations file (MDF), but they are not applied unless this parameter is set to 2. Including rigid body motion affects the display or animation of the flexible component, but it has no effect on dynamic stresses.

Request stress/strain/displacement output for postprocessing (see the MSC.Nastran quick reference guide for more information):

An example MSC.Nastran input file for modal stress recovery run compared to a typical input file for building flex body is shown below. These examples are located in the following installation files:

Note that "plate.cmd" is the command file to create the example model with the flex body (MNF) by "plate.dat" and run the dynamic simulation.